Trying to get "relative view" of mitered skewed pipe in below weldment.....

I need to get a drawing of a skewed pipe with miters on both ends out to shop but since this pipe is kicked in both directions, I am having trouble trying to get a nice view of it on a drawing. I was thinking of making a reference plane along the 3d plane but not sure how to get the plane made. If I bring just the pipe onto drawing view, it is kicked and not true to the length I need (the 3d line is 34.72 in length so my pipe should be around that). Am I on the right track of needing a ref. plane developed that I can pick when using "relative view" of the pipe once within the drawing? I've also attached the .sldprt. Thanks in advance!

I created a sketch on the surface of the W-section. I started with a rectangle, then made each side tangent to the pipe edge, and one of the long sides parallel to the pipe's axis to fully define it. I then placed points coincident with the midpoints as you see below. I then created a Plane coincident with one of these points and the pipe's axis. I clicked on this plane and clicked the Normal To button to orient the model normal to the plane and created a new view. I then used this view in a drawing, showing only the pipe with the Select Bodies button.

Instructions for saving and placing the views are in #15 here: Frequently Asked Forum Questions . It seems like there should be an easier way to do this, but this is the best I could come up with.

Ahh, it was created along with the structural member automatically. That's why I didn't see it. When you say "separate the component from the frame" do you mean "insert into new part"? That's what I did to keep it by itself as a part linked back to original but I don't see Plane9 in there now, just the "stock" note in FMT. I'm assuming that your suggestion is all within the part itself correct (not within the drawing). I hate to have all these questions the last few days but trying out new things in SW recently (I'm sure various questions from members keep all of you experts sharp!)

I actually had almost exactly what you have shown but didn't think it looked right. I just made a new config with everything hidden but the pipe. It appears that the miter on the pipe is not in line on near side / far side like the shop foreman and I were thinking. We were both thinking that this miter would be straight thru if looking normal to the pipe (like a front view as in your first pic above (not on a skew)). Gotta love SW to prove that its not.

It appears the miters are indeed parallel to each other. If you take my top view and rotate it the ellipses go away and straight lines appear. What I am saying is I think if this part was to be cut on a mitered cold saw, the second cut could easily be gauged off the first with a stop perpendicular to the table. Hope that makes sense.

That does make sense. Matches with what Ken had attached as well with a simple pipe cut with parallel miters end to end. Should just be able to cut on our saw which can go 45 degree either way off vertical with the table horizontal.

I created a sketch on the surface of the W-section. I started with a rectangle, then made each side tangent to the pipe edge, and one of the long sides parallel to the pipe's axis to fully define it. I then placed points coincident with the midpoints as you see below. I then created a Plane coincident with one of these points and the pipe's axis. I clicked on this plane and clicked the Normal To button to orient the model normal to the plane and created a new view. I then used this view in a drawing, showing only the pipe with the Select Bodies button.

Instructions for saving and placing the views are in #15 here: Frequently Asked Forum Questions . It seems like there should be an easier way to do this, but this is the best I could come up with.

Tried your method first. Attached is the .sldprt. When I bring into new drawing and "select body" to get only the pipe showing and set to view DMK (which is new view i made normal to Plane 13), I get a skewed view. See snapshots below (first two for part; second is normal to view DMK). Last snapshot for drawing showing it skewed. I believe I did what you suggested. I would need to rotate the view to get the straight thru miter like you show on your second shot though (looks like yours is rotated to miters are in line).

Attachments

Go back and look at my screenshot again. You need to edit the sketch and place a point at the centerpoint of one of the short sides of the rectangle, trhen use this point to create your plane, not one of the corner points. I'd post my model, but I'm using a newer version and you wouldn't be able to open it.

I manually rotated the drawing view down and my view matches pretty close to Ken's from post below. I'm good with this. Thanks to all for your help. Much appreciated. Hate to bother all you experts but that's how we all learn. I'm sure we were all in the same boat at one point or another. have a great weekend everybody!

Glad to help. By the way, when you first brought the drawing view into your drawing it looks like the cut was horizontal, so you should have been able to use the angle of that cut to determine the amount the view needed to be rotated so the pipe sides would be perfectly horizontal. Maybe that's what you did, but it looks like it may be off just a little bit (not that it matters).

When I first brought it in, the miter was horizontal. I did EXACTLY what you said to bring the walls horizontal for the saw operator. Was just saying I would have though the Align feature would have worked by selecting the lines running parallel to axis and clicked to make them horizontal instead of miter lines. Didn't work so I did what you said. My length measured what Ken came up with to the tee (I originally said it was a bit off till I noticed the one point grabbed the inside wall instead of outside).

Attachments

You can cut the one end on the saw no problem, however some how you need to clock it or mark the pipe in a way that the guy cutting know how far to turn. There are different ways to do this, however you would need to find out from the shop floor how they want to see it on the drawing, otherwise you could be just confusing them.

edited

Dave I missed saying if the angle isn't the same on both ends, yes I did see that your part had the same angle.

I have often placed a part like this in my drawing even if they are skewed, pick the one view and draw a vertical line and measure the amount of angle then turn the part by that many degrees and then pull the other views off of that view. In your case here I think the part would go both directions which creates another matter.

Like I said all you need to do is select Plane and hit normal to and go from there

Since you have coplanar cuts this is fairly easy. Make a new configuration call it "drw" Update your cutlist folder. Now grab the body that you want to detail and add a "move-copy" feature using constraints. Add one tangent constrain with the round tubing face and the top plane, add another coincident constrain using one of the cut faces and the front plane. Now you have your body aligned with the main planes of your weldment part. Create a drawing, select the body that you added the move-copy command and select a standard orthogonal view from the pick list. you can dimension the angle, length etc. easily.

Bonus, after the design change, the view will always be aligned due to the move feature. Note, you need to suppress the move command in your design configuration.

One thing to keep in mind Dave.... One way is.... All 2D sketches are developed on a plane or a surface and that is the "Normal To" plane where you can add new views or anytime you work with skewed pipe and you see your going to sketch on a face you can always add four sketch points quadrant to the circle, then like Glenn mentioned, add a plane by selecting three of the four points and use that for your new views....

Or you can add a 3D sketch and select the outer edge of each end and convert the entities add additional sketches to find the center, then you can add a construction line from end center point to end center point, now you can choose that line and an end point to insert a plane. I would only do this if there 2 non parallel faces of contact and also that the pipe would go on an angle, creating two entirely different compound angles.

I did create a sketch like Glenn suggested at the lower end of the pipe (rectangle with all four sides tangent to quadrant points on ellipse). Then made a point at the one line coincident with quadrant point of pipe. Was curious though why I just couldn't have created a reference plane using the pipe axis as one selection and the point at the quadrant without having to go thru the exercise of making the whole rectangle (I believe only one point was needed off the rectangle along with the axis to create the plane).

I did create a sketch like Glenn suggested at the lower end of the pipe (rectangle with all four sides tangent to quadrant points on ellipse). Then made a point at the one line coincident with quadrant point of pipe. Was curious though why I just couldn't have created a reference plane using the pipe axis as one selection and the point at the quadrantwithout having to go thru the exercise of making the whole rectangle (I believe only one point was needed off the rectangle along with the axis to create the plane).

I tried that, but couldn't get a sketch point fixed at that point of the pipe quadrant without creating the rectangle first. If someone else was able to do this I'd be happy to hear how they did it.

Yes, agreed Glenn. I tried that too lol and had no luck but figured I goofed something up. I also tried just sketching one line tangent to that area of pipe and make a midpoint of that line coincident to the quadrant point of the pipe and then sketch a point on the midpoint of that line but it said I cannot put a point where there already is a point. But there was no point to pick when I tried to find one on ellipse quadrant when creating the plane. Who knows.....

Interesting Dennis. So to create the reference plane, we just could have picked that little quadrant point as one selection and the pipe axis line for the second and that should have created the plane right? I couldn't "find" that darn point and apparently neither could Glenn Have a nice holiday.

That's it Dave,, You might want to use the quadrant snap (I have the snap tool bar visible) to assist in this. This is the method I use in my second pic in my first post in order to get plane 1. Then you can make a plane perpendicular to that (also using the axis) for a top plane.